Arduino Diecimila gridded ground plane + EMC

Hello all, I would like to know how the Arduino Diecimila fairs from a EMC/EMI point of view. Unless careful PCB design is used, microprocessors can radiate nuisances levels of EMI.

A ground plane is the usual first starting point to control EMI and I notice the Arduino Diecimila has a gridded ground plain on the top surface, but could someone who owns one say if there is a similar gridded ground plain on the underside please?

I have looked at: http://www.arduino.cc/en/uploads/Main/arduino-diecimila-reference-design.zip with Eagle, but this the early version without the ground plane so I cannot find out that way.

I have looked at: http://www.arduino.cc/en/uploads/Main/arduino-diecimila-reference-design.zip with Eagle, but this the early version without the ground plane so I cannot find out that way.

My copy of that "reference design" has ground planes on both top and bottom. Did you remember to do "ratsnest" after opening the board in EAGLE?

In the course of the Freeduino PCB layout, there were some interesting discussions about minimizing EMI and such. One of the comments was that having ground planes on both sides was not necessarilly considered helpful in that respect. There are a couple aspects of the freeduino layout that are supposed to "improve" EMC (guard ring around the crystal signals, some attention to the return path for bypass caps) , but they are derived from hearsay without measuring either the original deicimila to see if changes were needed, OR measuring the new board to see if the changes helped any. (and I am by no means experienced in EMI-minimizing PCB design.)

(of course, it is a nice feature of open-source hardware that you can take the reference design(s) and tweak it yourself for lower EMI, if necessary...)

there is a ground plane on both sides

it is gridded because during the production phase it saves energy and provides a more even distribution of metal in the holes and vias.

on the other hand on of the best things with arduino is that with 20EUR you get one and you can test as much as you like...

m

Thanks for the responses.

I agree that at 20 euros you cannot go wrong, but for the moment I would like to comment on Eagle and westfw’s comments.

Yes, when I pressed the Ratsnest button the grid ground plane was constructed, but why did that happen when the gnd net were already routed?

Ok I turned off the option ‘Ratsnest Processes Polygons’ and pressed Ratsnest again on a virgin file and this time the grid ground plane was not constructed.

Why did Eagle create a grid ground plane on the gnd net and not on Vcc for example?

I am confused as how Eagle can do this and have searched the Internet but so far have not found a reference to Eagle performing this function , can anyone enlighten me please?

BTW I have designed a PCB with Protel in the distant past so am familiar with the concepts from schematic to gerber, but I didn’t manage to get Protel to create grid ground planes like Eagle just did! :o

Im not really understanding the question but Ill take a stab at it…

To create a power plane in eagle the easiest method is to use the text command “poly” followed by a space and the net name for the plane such as “gnd”. This is the easiest way to attach a polygon to a power net because once named it will not let you rename the polygon to anything else. So if you wanted to create a power plane attached to vcc the command would be “poly vcc” and enter to evoke the command.

Once the command is evoked you have the option to define the layer (top or bottom), the width of the trace that will compose the plane, whether the pour is solid or hatched (the “gridded plane” in your question), and a few other options.

It is possible to use the change command to change the pour from solid to hatched. IIRC Eagle will by default make all polygons solid so unless this was defined by the designer a plane will show up as solid. Some of the arduino files have solid planes but I just assume that is a fluke or they are older files.

It is also possible to have a hatched plane that appears solid. This would be because the spacing has to be set to greater than the trace width in order for there to be space or gaps in between the traces. Once the poly is drawn all these options can be changed by the change command.

Personally I almost always use hatched power planes partly because as Mossimo said, I understand them to be better physically for the board but also because Im an artist I am simply more attracted to them aesthetically. I usually dedicate one plane to vcc and another to gnd just to make things easier. I also avoid traces or planes under oscillators as I understand this too helps with EMI. In the end though even at 16mhz this isnt rocket science nor is it that high speed of an application that it matters much to the actual user.

Best,
Brian

Thanks for the responses.

I agree that at 20 euros you cannot go wrong, but for the moment I would like to comment on Eagle and westfw's comments.

Yes, when I pressed the Ratsnest button the grid ground plane was constructed, but why did that happen when the gnd net were already routed?

Ok I turned off the option 'Ratsnest Processes Polygons' and pressed Ratsnest again on a virgin file and this time the grid ground plane was not constructed.

Why did Eagle create a grid ground plane on the gnd net and not on Vcc for example?

I am confused as how Eagle can do this and have searched the Internet but so far have not found a reference to Eagle performing this function , can anyone enlighten me please?

BTW I have designed a PCB with Protel in the distant past so am familiar with the concepts from schematic to gerber, but I didn't manage to get Protel to create grid ground planes like Eagle just did! :o

While adding the polygon to create the plane, you can associate it to a NET name. Usually you write GND and the ground plane is created. I have not tested with different planes, but I assume it gets associated to the NET name you specify while creating the polygon.

Thanks for the advise, I now understand and have now spotted that on the reference design Eagle .brd there are the GND polygons already drawn on the top and bottom layers enclosing the whole PCB, so the Ratsnest command did what was expected of it.

These learning curves with new software packages... ::)

This is the easiest way to attach a polygon to a power net because once named it will not let you rename the polygon to anything else.

Not so: select name tool, click on part of the border of a poly as if it was a normal track and viola, renamed poly :)

If you move a corner of a poly, it'll "undraw" it so you can see its borders more clearly.

If you move a corner of a poly, it'll "undraw" it so you can see its borders more clearly.

Much easier and less destructive is to use the 'rip-up' tool on the edge of a polygon.

This link has a tutorial on adding a ground plane http://tangentsoft.net/elec/movies/tt10.html

One thing I noticed is that orphans are enabled for the ground plane. Usually that's a bad idea from an EMR perspective because unconnected pads act as passive radiators and capacitor plates rather than ground.